Stats

  • Replies 4
  • Subscribers 48
  • Views 18896
  • Members are here 0

Missing .lib files?

Sarkreth

Hello,

I'm trying to simulate a fairly simple two-BJT amplifier, which uses MPSA18 transistors, which I found with the "transistor.olb" library. When I try to simulate, though, I get these:

WARNING(ORNET-1119): No PSpiceTemplate for Q1, ignoring

WARNING(ORNET-1119): No PSpiceTemplate for Q2, ignoring

I suspect this is because there is no corresponding "transistor.lib" file in my C:\OrCAD\OrCAD_16.5_Lite\tools\pspice\library folder. In fact, there aren't nearly as many .lib files as there are .olb files.

Is there somewhere I can find the library(ies) I need, or am I doomed to a limited number of models since I'm using the Lite version of Capture? Or am I having a completely different problem? Thanks a ton.

  • oldmouldy
    You are using the Lite version so, strictly, only the parts in the EVAL.OLB and models EVAL.LIB are supported. You could try adding the Bipolar.olb from the tools\Capture\library\PSpice directory and place the part from there. Then Edit the Simulation Profile, Configuration Files tab, Library selection on the left, use the upper Browse button to locate the Bipolar.lib from the tools\PSpice\library directory, select this and then use the "Add to Design" button to add the simulation models. Note that, since you have a Lite version, you may need to add the LIB file back to the Simulation Profile each time that design is opened before the simulation is run since the configuration may be reset for the Lite installation.
  • Sarkreth

    Well, I don't appear to have a Bipolar.lib file, so I can't directly take your suggestion.

    However, I've found this: http://network.wenzel.com/misc/spice.htm which does appear to have a model for the part I need.

    I've made a Trasistor.lib file from it, put it with all of the other .lib files, and added that to the design, but I still get the same error.

  • oldmouldy

    The issue is that the Schematic parts that you placed are from the general purpose libraries and therefore don't have the necessary properties to make a PSpice netlist, specifically, but not exclusively, the PSpiceTemplate property, hence the message. This property maps the Schematic pin names on the Schematic part to the Pin Order on the model. For a .MODEL defined transistor, this would be:

    Q^@REFDES %c %b %e @MODEL

    The Schematic Part Pin Names would need to be c for the Collector, b for the Base and e for the Emitter for this template to work. You also need an Implementation Type property of PSpice Model and an Implementation property of the Model Name, MPSA18 in this case.

    See the PSpice Users Guide, pspug.pdf in the doc\pspug directory of the installation for details. The "Lite" version has restricted Model Editor capabilities so you probably won't be able to use this to make a Library from the LIB file that you have.

CDNS Forum Thread CSS JS
CDNS - Fix Layout